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Not really, but you could select some geometry belonging to the part you want within the DrawingView, then get the document that geometry belongs to within the code after the selection. Or you could navigate the BrowserNode for that view, to get the part you want, either manually or by code. You could also probably pop-up an InputListBox with the list of all parts within the assembly, and select one that way. If you want to select the part completely by code, instead of using the Pick method, you would have to specify something about the part you want, so it can find it.
Wesley Crihfield
(Not an Autodesk Employee)
FYI: You can set the Part Priority selection preference by code but it just doesn't work with the Pick function.
Dim oDDoc As DrawingDocument = ThisDrawing.Document
oDDoc.SelectionPriority = SelectionPriorityEnum.kPartSelectionPrioritySame for the SelectionPreferences property of the DrawingDocument.
You can set it to select specific type of object, but the Pick function has it's own filter settings, which override these settings.
Dim oDDoc As DrawingDocument = ThisDrawing.Document
oDDoc.SelectionPreferences.Add(ObjectTypeEnum.kPartComponentDefinitionObject)There are other ways of selecting things though.
Here's a 'somewhat' simple example of the method I mentioned before. This iLogic rule will get the model document being represented within the specified view, then if it is an Assembly, it iterates through all its referenced documents, checking to see if they are Parts, then and adds their FullFileName and PartDocument object (key - value pair) to a Dictionary object for temporary storage. When the loop finishes, it presents you with an InputListBox of the FullFileName's of those Parts. You can select one, then the code gets the corresponding PartDocument. Then I just added a MsgBox at the end to show you the FullFileName of the new PartDocument variable, to show that it worked.
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("This rule '" & iLogicVb.RuleName & "' only works for Drawing Documents.",vbOKOnly, "WRONG DOCUMENT TYPE")
Return
End If
Dim oDDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Sheet = oDDoc.ActiveSheet
Dim oView As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter,"Select a View.")
Dim oParts As New Dictionary(Of String, PartDocument)
If oView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
Dim oADoc As AssemblyDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
For Each oRefDoc As Document In oADoc.AllReferencedDocuments
If oRefDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim oPDoc As PartDocument = oRefDoc
If Not oParts.ContainsKey(oRefDoc.FullFileName) Then
oParts.Add(oPDoc.FullFileName, oPDoc)
End If
End If
Next
End If
Dim oPartName As String = InputListBox("Select the part document you want.", oParts.Keys, " ", "PARTS")
'MsgBox("You chose: " & oPartName)
Dim oPartDoc As PartDocument
oParts.TryGetValue(oPartName,oPartDoc) '<<< This line just set the value of the oPartDoc variable
MsgBox(oPartDoc.FullFileName)Wesley Crihfield
(Not an Autodesk Employee)
Hi @Rob987654
Try this iLogic rule to pick a part in assembly drawing.
To show that an occurrence is selected it will return its name 🙂
Sub Main Dim oSelect As New clsSelect oSelect.SelectOccurrence(ThisApplication) Dim oOcc As ComponentOccurrence = oSelect.SelectedOcc oSelect = Nothing MsgBox(oOcc.Name) End Sub Class clsSelect Private WithEvents oInteractEvents As InteractionEvents Private WithEvents oSelectEvents As SelectEvents Private bTooltipEnabled As Boolean Private ThisApplication As Inventor.Application Public SelectedOcc As ComponentOccurrence Private stillSelecting As Boolean = True Public Sub SelectOccurrence(oApp As Inventor.Application) ThisApplication = oApp oInteractEvents = ThisApplication.CommandManager.CreateInteractionEvents oInteractEvents.InteractionDisabled = False oSelectEvents = oInteractEvents.SelectEvents oSelectEvents.AddSelectionFilter(SelectionFilterEnum.kDrawingCurveSegmentFilter) oSelectEvents.WindowSelectEnabled = False bTooltipEnabled = ThisApplication.GeneralOptions.ShowCommandPromptTooltips ThisApplication.GeneralOptions.ShowCommandPromptTooltips = True oInteractEvents.StatusBarText = "Select component" oInteractEvents.Start() While stillSelecting ThisApplication.UserInterfaceManager.DoEvents() End While End Sub Private Sub oInteractEvents_OnTerminate() Handles oInteractEvents.OnTerminate ThisApplication.GeneralOptions.ShowCommandPromptTooltips = bTooltipEnabled oSelectEvents = Nothing oInteractEvents = Nothing stillSelecting = False End Sub Private Sub oSelectEvents_OnPreselect(ByRef PreSelectEntity As Object, ByRef DoHighlight As Boolean, ByRef MorePreSelectEntities As ObjectCollection, ByVal SelectionDevice As SelectionDeviceEnum, ByVal ModelPosition As Point, ByVal ViewPosition As Inventor.Point2d, ByVal View As Inventor.View) Handles oSelectEvents.OnPreselect Try Dim oCurves As DrawingCurvesEnumerator = DirectCast(PreSelectEntity, DrawingCurveSegment).Parent.Parent.DrawingCurves(DirectCast(PreSelectEntity, DrawingCurveSegment).Parent.ModelGeometry.Parent.Parent) Dim oCol As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection For Each oCurve As DrawingCurve In oCurves For Each oSeg As DrawingCurveSegment In oCurve.Segments If oSeg IsNot PreSelectEntity Then oCol.Add(oSeg) Next Next MorePreSelectEntities = oCol DoHighlight = True Catch DoHighlight = False End Try End Sub Private Sub oSelectEvents_OnSelect(ByVal JustSelectedEntities As ObjectsEnumerator, ByVal SelectionDevice As SelectionDeviceEnum, ByVal ModelPosition As Point, ByVal ViewPosition As Point2d, ByVal View As View) Handles oSelectEvents.OnSelect SelectedOcc = DirectCast(JustSelectedEntities.Item(1), DrawingCurveSegment).Parent.ModelGeometry.Parent.Parent ThisApplication.CommandManager.StopActiveCommand End Sub End Class
Jhoel Forshav
Download my free Inventor Addin - Hole Projector
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